Re: [CAD_CAM_EDM_DRO] tool change

mszollar wrote:

> I have a technical question; using CNC what is the best way to
> execute a tool change?
>
> In CNC programs the 1st tool is very easy because you can adjust the
> tool to the part then move to 0,0,0. A 2nd tool change is different
> because the new tool may be longer, shorter, etc. Additionally you
> would not want to change Z (or any other axis) in the process of the
> tool change (or certainly you would want the axis to read the same
> before and after)

This is what tool length compensation (G43) is for. Most CNC programs
have a "tool table" which holds the length and diameter of the tools
loaded (or used with) the machine. I have a system which I have gotten
used to, but it is quirky. My first tool is often a center drill. I made a
simulated spindle taper for measuring all my tools, see
http://pico-systems.com/preset.html for a look at that. I measure the height
of all the tools with a vernier height gauge, with the R-8 holders in the
presetting tool. I then write down this length and tell the machine
that this tool is length zero. This measured length is then subtracted from
all other tool lengths, and the difference is entered in the tool table.
So, with no G43 in force, I can work with the center drill, often by
bringing it down until it pinches a piece of paper against the top of the
workpiece, and then setting the Z axis to 0.005" (the thickness of the
paper). When the 2nd tool is called for, I have the program select the
length offset with G01 G43 H6 if the new tool is tool #6 in the tool table.
The first move of the Z axis will include this offset. So, let's say the
new tool is a drill, and 1.5" longer than the reference tool, the center
drill. And, let's say the first move is Z-.5, and that the reference tool was
left at Z=2.0" (that would actually have the center drill 2.0" above the work).
Now that the longer drill is in the spindle, it is only 0.5" above the work,
and we will be requesting it to drill 0.5" into the work, so we only need it to
advance 1".
When it executes the Z-.5, it will only advance one inch, because the
offset will be applied. (If you forget to set the tool length in the table, or
forget the G43 Hxx in the program, the tool would drill 2" into the work.
I have done this a few times, too.)

The reasoning behind all this craziness, is that I can also keep track of
something like quill position, so that I can arrange things such that when the
offset is removed with the G49, and then a Z2.0 or something is commanded,
the quill will get returned pretty close to full up position. I have to change
tools manually, so that is convenient. I suspect there are other ways to do
this, and if you really have an auto tool changer, then keeping the tool
length offset in force all the time might be better.

I hope this makes some sense. Once you've done it a few times, it becomes
familiar, but the first couple of times, you really bite your nails.

Jon